Tetra Meshing

Use the Tetramesh panel to fill an enclosed volume with first or second order tetrahedral elements. A region is considered enclosed if it is entirely bounded by a shell mesh (tria and/or quad elements). Other element configurations generated in this panel are: hexahedral, wedge, and pyramids. These elements are typically generated when you need boundary layer type meshes on certain areas of the volume surface.

The following subpanels exist for different types of tetra meshing:

Subpanel

Description

Tetra mesh

Fills an arbitrary volume, defined by its surface using tria/quad elements, with tetrahedral elements.

Tetra remesh

Regenerates the mesh for a single volume of tetrahedral elements.

Volume tetra

Given a solid entity or a set of surfaces representing a closed volume, this meshing option generates a shell mesh and fills the enclosed volume with solid elements. You can choose to create a shell mesh (2D) using quads, trias, or mixed elements and a solid mesh (3D) using tetrahedral elements only or mixed (tetras and penta) elements. In addition, you can use proximity meshing, which refines the mesh in areas where the features are small and closer together. See the following examples.

tetramesher1

You can also use surface curvature as a function of element density as shown below. This option creates finer mesh in areas of high surface curvature.

tetramesher2

When you select quads or mixed as your 2D element type, HyperMesh creates quad elements and splits them diagonally into two trias during tetra face creation. This can create tetra elements whose triangular faces are right triangles (90-45-45 angles) instead of equilateral triangles (60-60-60 angles).

tetramesher3

Note:

Sometimes the meshing may fail to correctly interpolate from the surface mesh; when this occurs, the shell elements are cleaned up according to the same settings used in the Quick TetraMesh macro on the Utility Menu, and a second attempt is made. This means that some of the features in a model may be smoothed over.

Tetramesh parameters

Sets general qualities of the tetrameshing engine, such as a maximum element size, growth rate, the balance between speed and element quality, or whether to perform smoothing operations after initial meshing.

Refinement box

Lets you define a specific box-shaped volume within an existing teramesh in which to generate finer mesh.

You can specify some elements to be fixed, and others to be floatable. A fixed tria-quad element is one that must be exactly represented as a face of a tetra/penta-pyramid/hexa element in the final mesh. A floatable element is one whose nodes locations are used, but the exact connectivity of those nodes can be modified if it produces a better mesh. Unless you need a special mesh type (such as surface layers of pentas/hexas), you should select as fixed only those elements that must match a pre-existing mesh, leaving the rest floatable. If the bounding surface contains quad elements, and if these quad elements are defined as fixed elements, then a first layer of elements is generated on the boundary, and pyramid elements are generated from the quad faces. However, when quad elements are defined as float elements, they are split into two trias, and the tetra meshing proceeds normally.

You can also specify various growth options in order to control the tradeoff between the number of tetras generated and their quality. Higher, more aggressive growth rates produce fewer elements, but they may be of poorer quality.

In the Tetramesh panel you can choose from three different mesh generation priorities. The generate mesh normally option applies in most cases, but if your solver is particularly sensitive to element quality, use the optimize element quality option. This directs the tetramesher to spend more time trying to generate better quality elements. In particular, it employs the volumetric ratio (CFD "skew") measurement for rating potential tetras. For some applications, element quality considerations are less important than mesh generation time. In those cases, choose the optimize meshing speed option.